3-D CAD: Unfolding problems
Dealing with a misplaced modeling technique
Columnist Gerald Davis provides some tips on getting that 2-D drawing--derived from the 3-D model--to manufacturing in the best shape possible.
We start with the usual disclaimer that we’re examining functionality that is unique to SolidWorks®. In this article we discuss some of the opportunities of history-based modeling as it relates to the automatic unfolding of sheet metal models.
Consider a scenario that puts us in the role of generating a flat-pattern file for importing into a CNC programming system. This process is essentially two operations—creating the flat layout and creating the file that contains the flat-layout information. The modeling software I use will unfold a properly modeled part automatically. It also will export 2-D data in several formats, including the popular DXF file format.
Although the production of flat layouts is frequently beyond the area of responsibility for 3-D CAD modeling professionals, those modelers should take steps to ensure the manufacturing process is a seamless integration that avoids duplication of effort. Be kind to your CNC programmer! Whenever practical, model using a material thickness, K-factor, and bend radius that your manufacturing team approves. If in doubt, a simple e-mail will get you the information. Given the right settings, the generated flat will be exact.
Several Internet resources provide excellent information about flat layouts. The Web site www.sheet metalguy.com should serve as an inspiration for additional Web searches. His method of flat-layout calculation is not the only one that works.
The Dangerous CAD Jockey
Back to our scenario. Our customers love the convenience of just sending 3-D CAD models to us and leaving all of the drafting in our hands. Our hypothetical service transfers a lot of responsibility to us, so we must always be cautious about making changes to the 3-D model. Don’t inject edited models into a manufacturing process without permission. Make sure you keep original copies safe and secure for reference. Confer with the originating designers to make sure you are not creating a monster with your good intentions.
Outside of the CAD world, making a flat layout consists of calculated plotting and verification of the calculated plot. The verification of the flat layout—using the specifications for the finished part as the controlling document—is vital to success. The “specifications” are traditionally delivered as drawings printed on sheets of paper with projected views in accordance with industry standards.
The most labor-intensive solution for the production of the flat layout is to redraw an appropriate 2-D profile manually based on the projected views while using the correct bend compensation for proper sizing. A less labor-intensive solution is to have the 3-D CAD editor export a perfect 2-D flat layout for the part in question. I’m a fan of efficiency, so let’s use the automatic approach.
No matter how the flat layout is produced, it needs to be checked against the original specification to eliminate errors and omissions. The primary advantage of the CAD-generated flats is that proofreading someone else’s work—in this case, the computer’s—can have a higher success rate than double-checking your own lengthy list of tedious math and mental interpretation of a 2-D drawing of a 3-D part. Which begs the question, “What could possibly go wrong with computer-generated flat patterns?”
A Vanishing Case Study
In Figure 1 a 3-D CAD model for a bracket that we’ve inherited is shown. The goal is to make a flat pattern for CNC production. The CNC programming department has requested that the flat layout be delivered to them in a DXF file format.
Let’s study the process of exporting the flat pattern for the part shown in Figure 1. In Figure 2a, you’ll note that the Flat-Pattern1 feature is highlighted in the Feature Manager’s history list. The first step in exporting a flat-pattern DXF file is to right-click your mouse on the Flat-Pattern1 feature.
To complete the Export Options dialog options properly, you need information about the target system—the software that will be importing the DXF file. You might run a few test cases with various options to verify that no versioning conflict between 3-D CAD and 2-D CNC prep exists. I’m not going to cover all of the options here, but I recommend that you read the information found in the Help system to learn about settings that are useful for exporting DWGs to other CAD systems.
Referring to the Export Options dialog box in Figure 2c,
- For the software Version, selecting a primitive/ old version is reasonable. However, if the part is curvy with polylines and splines in the geometry, then newer versions are prudent. Note additional options for dealing with splines are presented later in the dialog.
- The Fonts options can be important if you are exporting finished DWG drawings, artwork for screen printing, or other profiles where the font is critical. Font is not routinely important to flat layouts.
- The Custom Map Enable allows you to include forming tools, bend lines, and other nifty items in the DXF. Once you’ve settled on a mapping preference, including layers and colors, you can save those preferences in a map file. With the proper map file and warning settings, the DXF export process can be automated and streamlined. For routine flat exports, you don’t have to mess with the mapping; the imported DXF will just be black and white with everything on layer 0. For this instruction, it’s enabled. You might find it more convenient in production to leave this disabled until you find the need to set up a map file to automate your preferences.
- End Point Merging is something I usually disable unless I know I need it. This deals with sketch entities that appear to touch but don’t quite—some little gap in the millionths of an inch range. If the CNC programming system is confused by lines that should be connected but are not, then try Enable Merging and set a limit range that won’t accidentally distort the layout to be out of an acceptable tolerance range. If you’re hoping for ±0.010 inch, then set your merging range to 0.001 as a starting point.
After saving or canceling this review of export preferences, let’s go back to Figure 2b. It’s time to give the exported DXF a meaningful file name and click on the Save button. That leads to Figure 2d —the DXF/DWG Output dialog.
Here’s a review of some of the settings in the DXF/DWG Output dialog:
- For a 2-D flat-pattern export, Sheet Metal is the best choice.
- Under Entities to Export, you might find the Bend lines option to be great for 1:1 templates—helpful for forming transition ducts, for example, and terrible for everything else. The Forming tools option can be interesting too. Without this enabled, you may find that forming tool features disappear from the flat layout, which you may or may not like. Once the settings are pleasing to the manufacturing department, take the time to create mapping files—or memorize these settings in some alternative manner.
- Under Output Alignment, esoteric considerations like grain direction in the material can be dealt with. Maybe the target CNC system is so antiquated that it has to have the same part of the profile located at coordinate point (0,0). This is where you can fine-tune the export for those unusual situations. Nearly all CNC programming systems in use today have better tools for nesting the part in the blank. You may never have a need for managing the Output Alignment. At least you know you have the power when and if you need it.
After clicking on the Green Checkmark to accept the displayed settings in the DXF/DWG Output dialog, a DXF/DWG Mapping dialog, as shown in Figure 2e, is next.
Mapping Layers and Line Types
The SolidWorks to DXF/DWG Mapping dialog allows you to define layers, map entities, and map colors so that the result in the target system more closely matches the appearance as viewed with SolidWorks. You might be tempted strongly to disable the mapping options when generating flat DXFs, which is certainly my habit. However, I wanted to drag you through all of these options so you might discover that magic option that simplifies your workflow, particularly when exporting drawings to other 2-D CAD editors.
In the case of a flat layout, a CAD jockey doesn’t have much to map in the way of layers and line types, so click on OK. This will launch the DXF/DWG Cleanup tool.
“Dirty” DXFs have lines on top of lines, dashed lines around hardware holes, and other sketch entities that merely confuse the CNC programming effort. This Cleanup tool does a fine job of prepping the flat pattern for generating a tidy DXF.
Figure 2f shows an example of the DXF/DWG Cleanup tool. This is a preview of what the exported DXF will include. You’ll recall that I included Bend lines in my output options (see Figure 2d). To remove a bend line—or any other sketch entity—select and then click on the Remove Entities button. Repeat until satisfied. Then, with a mouse click on Save, SolidWorks will proceed with the creation of a DXF file containing a 2-D flat layout of the sheet metal part.
As a side note, a different technique for creating DXF flats is available. That process involves creating a drawing—a slddrw file type—that includes a flat view of the part and then saving that drawing as a DXF. The slddrw could include layers, colors, and line types that are not available in the direct flat-DXF export technique.
And, as a bit of reassurance, generating a flat-pattern DXF is not very hard. The default settings usually work just fine.
Look, Ma! No Holes!
At the end of the export process, my vanishing demo part gets rebuilt. The result is shown in Figure 3. The disappearance of the slots is not a flaw in the software, but rather is a result of the modeling technique that was used to create this demo part.
Note in Figure 3 that Cut-Extrude1 is a child of Flat-Pattern1. It appears after Flat-Pattern1 and has some feature that is associated with Flat-Pattern1. By default, all children of a parent will follow the suppression of the parent.
The DXF flat-pattern export process, in order to flatten the part, unsuppressed Flat-Pattern1. As a consequence, its child Cut-Extrude1 also was unsuppressed. That had no apparent impact on the slots in Cut-Extrude1 because they started out in an unsuppressed state. As the export process completed, it returned the Flat-Pattern1 feature to the suppressed state. As a consequence, the Cut-Extrude1 also was suppressed. That’s why the slots appeared to disappear in the model.
Finding Fault With Fixing Flats
What to do about this weird model depends on your area of responsibility. It is conceivable that you’ve created the flat-pattern DXF file and that’s enough. The fact that the slots are vulnerable to unexpected suppression might not be something you need to correct.
Suppose, however, that you’re also responsible for creating the shop drawings for the part. That means that at least you need to get the slots back into an unsuppressed state. Let’s go all the way and suppose that you have authority and responsibility to correct the model so it doesn’t have vanishing holes.
The first step is to consider why Cut-Extrude1 was modeled as a child of Flat-Pattern1. Somebody might have a rational reason why a feature—like a cutout—would be expected only in a flat configuration of a part. We could speculate on reasons why various configurations of a model would include or exclude features. Instead, let’s presume that Cut-Extrude1 should not be a child of the Flat-Pattern1.
In this bad demo model, we’re lucky. All we have to do is click-and-drag Cut-Extrude1 up the history list so that it appears anywhere prior to Flat-Pattern1. Right after Base-Flange1 might make sense. In a more complicated example, a CAD operator might have to delete some sketch relations to reorder the feature in the Feature Manager’s history list.
The names of these features were generated automatically as I created them. This gives you a strong hint about how I created this bad example. In the real world, this problem under discussion might be a consequence of an accidental dragging with the mouse.
Even though the reordering of features in the Feature Manager’s history list appears to have succeeded, the slots won’t reappear until Cut-Extrude1 is unsuppressed as shown in Figure 4 .
As a test of the repair, we click on the Flatten icon (see Figure 5a ). The part unfolds because the processing of bends is unsuppressed, and all the holes are shown as expected. Figure 5b shows the unclicked Flatten icon with the part folded and all the holes. The part appears to be folded because the processing required to unfold the part is suppressed.
Now that the part is modeled so the cutouts persist regardless of the flat/folded configuration of the part, it’s possible to proceed in making the shop drawing without problem as shown in Figure 6. Note that the figure includes both a flat pattern and a formed part as demonstration that the “correction” made to the model was the right thing to do.
Gerald would love to have you send him your comments and questions. You are not alone, and the problems you face often are shared by others. Share the grief, and perhaps we will all share in the joy of finding answers. Please send your questions and comments to email@example.com.
The FABRICATOR is North America's leading magazine for the metal forming and fabricating industry. The magazine delivers the news, technical articles, and case histories that enable fabricators to do their jobs more efficiently. The FABRICATOR has served the industry since 1971.